Mesh Creation in StressCheck

To access mesh creation tools in StressCheck, select Class > Mesh or navigate to the Mesh tab in the Input dialog. The set of options under the Mesh tab provide for the specification of the solution domain using nodes and elements (i.e. the finite element mesh). Additionally, contact zones may be created for multi-body contact analysis, fasteners/links for modeling fastened connections in the Planar reference, and crack objects for crack path simulation in the Planar reference.

This functionality fits quite easily into the familiar Class > Action > Object > Method (C/A/O/M) command paradigm, and certain objects may be created in parametric form. The implementation supports the manual and/or automatic creation of mesh objects such as:

• Nodes: Global, Local, Point, Intersection, Projection, Offset, Mid-Offset.
• Standard Elements: Triangle (3-sided membrane), Quadrilateral (4-sided membrane), Tetrahedron (4-sided solid), Pentahedron (5-sided solid), Hexahedron (6-sided solid).

Mesh objects in StressCheck are distinct from geometry objects. This is because mesh objects are usually attached to geometry objects in order that the model will be parametrically and geometrically associative. Nodes are similar in definition to geometric points, in that they may be constructed by a variety of methods (global, local, offset, projection, etc.). However, only nodes may be referenced in the construction of elements.

Terminology

There are a few important terms and concepts that should be understood before navigating further:

• Node – A Node is a location in space which will be referenced in the definition of an element. A node may be defined using a variety of methods including: global location, attached to a local system, as an offset to a curve or surface, as a midpoint between two point-like objects (point, node, system), as a mid-offset between two point-like objects that are attached to the same curve or surface, as a projection of a point-like object to a curve or surface, as an intersection of two curves, or attached to a point. Nodes which have been attached to a point will automatically inherit the associativity of the underlying point and pass this information to elements which reference the node. Methods for creating nodes associated to underlying geometry include offset, mid-offset, intersection, intersect-multi, projection, and point (when the point used is associative to underlying geometry itself).
• Element – Elements are simply topological constructions used to represent the shape of a part. For this reason, users need only select an element based on its topology (shape). All other characteristics of the element are determined from the current reference system and theory, and from the user assigned attributes. In this manner, a single element definition may be used to solve a problem of elasticity or heat transfer, and may be used to perform a plane strain, plane stress, axisymmetric, or plate bending analysis. Elements are constructed by selecting previously defined nodes, or by the MeshSim automatic mesh generator. All elements constructed in StressCheck are geometrically associative, i.e. they inherit shape characteristics and assigned properties from underlying geometry. The level of associativity depends on the node creation methods:
  • If the nodes used to construct an element are associative to geometry, the elements will inherit the characteristics of the underlying geometry.
  • If the two nodes of an element edge are attached associatively to the same curve or surface, the edge will be mapped directly from the associated curve or surface.
  • If all the nodes of an element face are all attached to the same surface, that face will be mapped directly from that surface.
  • If one or more edges of a face are curved, but not all edges of the face are attached to the same surface, the face will be curved by performing a blending operation to produce a Coons patch representation for the face.
• Midside Element – StressCheck also supports midside elements (quadratic mapping). Quadratically-mapped elements can be created manually by identifying the vertex nodes, then drag individual edges to midside nodes to utilize quadratic mapping (Create>Edge>Midpoint). This new functionality makes it possible to automatically generate a mesh that has quadratically-mapped elements, and to later add or modify elements manually. When adding a new element, each edge of the new element that is shared with an existing element will automatically inherit the midside node from its neighbor. Beam, triangle, quadrilateral, tetrahedron, pentahedron, and hexahedron now support manual creation of quadratically-mapped elements. This enhancement also supports the connection of geometrically associative elements to quadratically-mapped elements.
  • Quadratically-mapped elements (6-noded triangles or 10-noded tetrahedron) are created in StressCheck when the default automatic mesh generator (MeshSim) is used. Quadratically-mapped elements may also be imported into StressCheck using the NASTRAN Bulk Data interface. Imported quadratically-mapped elements include the 6-noded triangle, 8-noded quadrilateral, 10-noded tetrahedron, 15-noded pentahedron, and 20-noded hexahedron.
  • These elements perform well in StressCheck as long as the polynomial level does not exceed 5 or 6 for unrefined meshes in curved features.
• Edge – An Edge is defined as the path between two nodes in the definition of an element. An element edge may be referenced in the definition of boundary conditions, and for post processing operations such as resultants, point extraction, 3D fracture mechanics, etc. Using the Move To action, a straight edge may be attached to a curve or surface by selecting the edge and dragging it to the desired curve or surface. Similarly, a curved edge may be converted to a straight edge by simply selecting it when the action is Move To.
• Edge Curve – An Edge Curve is a sequence of edges which are slope continuous. The tolerance used to determine continuity is 0.01 degrees by default. When the Edge Curve option is selected, a tolerance field will appear so that you may specify the degree of continuity. The Edge Curve option is convenient for specifying boundary conditions or performing post processing operations in order to avoid having to select each edge individually.
• Face – A Face is defined as the surface formed by neighboring nodes of an element. An element face may be referenced in the definition of boundary conditions, and for post processing operations such as resultants, point extraction, etc. Using the Move To action, a straight face may be attached to a surface by selecting the face and dragging it to the desired surface. Similarly, a curved face may be converted to a straight face by simply selecting it when the action is Move To.
• Face Surface – A Face Surface is a sequence of faces which are slope continuous. The tolerance used to determine continuity is 0.01 degrees by default. When the Face Surface option is selected, a tolerance field will appear so that you may specify the degree of continuity. The Face Surface option is convenient for specifying boundary conditions or performing post processing operations in order to avoid having to select each face individually.
• Explicit Associativity – The creation of geometrically associative mesh objects will create new explicit associative relationships in a model. For example, attaching a node as an offset, a mid-offset, or a projection to a surface or curve, or as an intersection of 2 or more curves. This explicit associativity will prevent the future application of a boolean or blend operation to a solid body. As a consequence, mesh objects should not be added to a body unless it is certain that no future boolean or blend operations will be necessary for the corresponding body (i.e. its faces, edges or vertices).

Creating New Mesh Objects

The options under Mesh provide for the meshing of the solution domain using nodes, standard element types, fasteners, links, contact zones, cracks, etc. Nodes and elements may be generated manually or automatically (via MeshSim automesh generators). As discussed in the Geometry Overview, StressCheck lets you separate the definition of geometric boundaries from the definition of the finite element mesh. Separation of geometric objects from mesh objects provides for a great deal of flexibility in modeling. Since boundary conditions may be attached to geometric boundaries, a geometrically associative mesh may be easily changed/re-meshed without affecting boundary condition definitions.

Note: with the release of StressCheck v12.0, manually generated nodes (and any elements meshed from these nodes) can be used to “seed” the MeshSim automesh generator. For example, nodes placed at specific intervals along a curve will be respected when the automatic meshing routine is invoked. Learn more details in MeshSim Automesh Generators.

Note: MeshSim automesh generated nodes and elements will automatically be geometrically associative, whereas manually meshed nodes and elements must be explicitly associated to geometry by using associative creation methods. Learn more about Node Creation Methods, Manual Mesh Generation, MeshSim Automesh Generators, and MeshSim Automesh Generation Methods. The following describes the creation of new mesh objects, automesh generators and automeshes via the C/A/O/M options in the Mesh tab.

Action Combo-Box

In order to create a new object by a specific method, you must first set the action to Create in the Action (first) combo-box of the C/A/O/M. Once the action is set to Create, the Object and Method combo-boxes of the C/A/O/M will automatically populate with the available options, and the Input dialog will provide more details about the expected inputs. Additionally, the mouse cursor will reflect the Create action (). The default when the action is set to Create is Create > Mesh > Auto (i.e. Global MeshSim automesh generator). The mesh object/automesh generator type can then be changed, followed by the creation method, by selecting new options in the Object and Method combo-boxes, respectively.

Data/Index Subtabs

At the bottom of the Mesh tab are two subtabs: Data and Index. The Data subtab allows for specification and modification of meshing input data (e.g. node X,Y,Z coordinates, node offset value, MeshSim automeshing parameters), while the Index subtab provides a scrolling list of existing mesh object/automesh generator records for selection, modification and deletion (Figure 2):

Note: the scrolling list of mesh object/automesh generator records in the Index subtab is determined by the mesh object/automesh generator type specified in the Object combo-box of the C/A/O/M. If no objects exist for the selected mesh object/automesh generator type, then the Index subtab will be empty. See the “Index Subtab Filters & Options” section below for more information.

To create new mesh objects, select the Data subtab at the bottom of the Mesh tab in the Input dialog, set the Action combo-box of the C/A/O/M to Create, and the Object and Method combo-boxes the desired mesh object/automesh generator type and creation method. Then, provide the meshing input data by screen selection of objects (if applicable) or by entering the input data in the available input fields (see below for more detail).

Index Subtab Filters & Options

The Index sub tab is specific to the Geometry and Mesh class tabs, and contains options for sorting, filtering and object ID lookups for the object type specified by the Object combo-box. For example, if the input class is set to Mesh and the A/O/M configuration is set to Select > Any Element > Selection, the following column options are available within the Index subtab (Figure 3):

• Columns may be sorted in ascending/descending order by clicking on the column headers.
• Right-clicking on the “#” column will display the “Go to ID…” button:
  • Clicking “Go to ID…” allows the user to enter a specific object number in the “Scroll to ID:” field.
  • Clicking “OK” will then scroll the user to the specified object number in the Index.
• Right-clicking on the “Type” column will display a filter option list for associated object types.
  • For example, if the Object combo is set to “Any Element” and the mesh contains Hexa, Penta and Tetra elements, the following filter option list would display on right-click:
  • By default, all object types are included in the Index rows (“All”).
  • Selecting one or more object types from the filter option list will include only objects of the selected object type(s) in the Index rows.
• Right clicking on the “Status” column will display a filter option list for object statuses.
  • The filter options are All, None, Selected, Hidden and Ignore:
  • By default, all object statuses are included in the Index rows (“All”).
  • Selecting one or more object statuses from the filter option list will include only objects of the selected object status(es) in the Index rows.

Screen/Text Input Toggle

By default, all input fields in the Input dialog are inactive and the checkbox above the input fields will read Screen:. Screen: assumes the model input data will be based on screen left-clicks or left-click + drag actions, with the inactive input fields reflecting the mouse cursor location/movement in the Model View (Figure 4):

For example, you may create a global node using Create > Node > Locate, with Screen: displayed and all input fields inactive. Then, hover your mouse cursor in the Model View and left-click establish the global X,Y,Z location of the node. Note all input fields populate based on the cursor location and movement. Individual input fields can be activated for manual text input by checking the corresponding checkbox next to the input field. All input fields can be activated by checking the checkbox next to Screen:. The checkbox label will change to Input:, and all input fields will be active for text input. Unchecking the checkbox will deactivate all input fields and the checkbox label will change back to Screen:.

Note: in some cases, it may be useful to leave one or more input fields inactive for screen input, and activate the remaining input fields for manual text input. As discussed previously, the inactive input fields will be populated once the mouse cursor hovers over the Model View, or a left-click + drag action is completed in the Model View.

Specifying Mesh Inputs

The meshing input data requirements will depend on the Object and Method specified by the user in the C/A/O/M combo-boxes. Some meshing input data will require screen selection (e.g. specifying a body for automeshing, intersection of two curves, a midpoint between two objects, selection of an object for projection to a boundary), entering the data into the provided input fields (e.g. node location, MeshSim automesher parameters), or a combination. When input fields are available, the input may be constant, parametric or formula-based. Note: input fields are currently limited to 15 alphanumeric characters.

Constant Input

Simply enter the value in floating point (e.g. 0.1) or scientific notation (e.g. 1e-1) in the input field. If the constant value is to be evaluated based on a simple expression, such as “5*0.1” then an “=” must precede the expression so it as written as “=5*0.1”. As shown in the below animation, hitting the tab key will evaluate the expression in the input field:

Parametric Input

Simply enter the parameter name, or an expression containing constants and parameter names, in the input field. Parameter autofill and validation check features are available as of StressCheck v12.0 to assist in parameter selection. For example, if there is a parametric model dimension (e.g. “dim1”) to be modified by a parametric scale factor (e.g. “scalefactor”), an expression can be written in the input field as “dim1*scalefactor”. Changing the “scalefactor” parameter value will result in an automatic model update, including a re-mesh if necessary.

If an input field has focus, using Alt+P will result in a popup containing a scrolling list of parameter names (Figure 5). Parameter names are not case sensitive. For more details on parameters, refer to Parameters & Rules Overview.

Formula Input

Simply enter the formula name in the input field. Formula autofill and validation check features are available as of StressCheck v12.0 to assist in formula selection. Valid formula names will appear in purple text, and are preceded by a pipe symbol “|”. No additional characters, such as “-“, should precede the formula name. To reverse the sign of a formula, or to scale the formula expression, modify the formula expression directly in the formula definition.

If an input field has focus, using Alt+F will result in a popup containing a scrolling list of formula names (Figure 6). Formula names are not case sensitive. For more details on formulae, refer to Formula Overview.

Node Creation Methods

Nodes should be thought of as topological objects that define connections between elements. Similar to Primitive Geometry Creation Methods, StressCheck supports a variety of node creation methods (associative and non-associative) for future element generation. They may be defined by a variety of methods: by global coordinates, by local coordinates, attached to a geometric point, as an offset on a geometric boundary, or as an intersection between two geometric boundaries, etc. These are all associative relationships. When you attach a node to a circle, the node definition “remembers” this attachment. If you later attach an element to a node which is attached to a circle, this associativity will be inherited by the element.

Associative Methods

• Intersection
• Intersect-Multi
• Offset
• Mid-Offset
• Point
• Projection

Non-associative Methods

• Locate
• Local
• Delta
• Point
• Midpoint

Learn more about Node Creation Methods. Note: the Point method will generate a geometrically associative node if the point is defined as an intersection between trimmed curves/surfaces. For example, if you attach a point to a boundary and then attach a node to this point, the node will inherit the association with the boundary, and the element attached to this node will automatically obtain a curved edge or face.

Repeating Nodes

When node objects are to be created at regular intervals (i.e. repeated), it can be helpful to make use of the Repeat function in the Input dialog (Repeat # =, as shown in Figure 7):

Note: the Repeat toggle is automatically switched off when the Accept button is clicked, but not when the left mouse button is clicked in the Model View. To repeat the creation of node objects using constant intervals, first toggle the input fields you wish to repeat (e.g. X:, Offset:). Then, check the Repeat #= checkbox. A “+” symbol followed by an interval input field will appear to the right each active input field. The Repeat input box will also be active, and you may enter the number of desired repetitions as an integer value (N). Next, input the initial values for the node object repetition in the left-hand input fields.  Enter the interval values in the corresponding right-hand input fields.

Note: leave interval values as “0” if you do not wish to modify the initial values. Below is an example of Create > Node > Offset with N=8, for creation of eight (8) nodes at 45 degree offsets on a wireframe circle object (Figure 8):

Left click on the wireframe circle, and eight (8) nodes will be automatically created at 45 degree offsets.

Note: the number of objects repeated should be equal to the value in the Repeat input box (N), with the first object created having the properties of the initial values and the last object created having the properties of the initial values + (N-1)*interval values.

Merging Nodes

The Merge button at the bottom of the Input dialog may be used to remove redundant and coincident nodes from the model. The program searches for nodes which are less than 10^-6 units apart. All but one of the coincident nodes are discarded, and all element definitions are updated appropriately. The tolerance for determining redundancy may be adjusted by supplying a parameter called “_merge_tol” with the desired tolerance value.

WARNING: Using Merge when the model has an intentional crack causes the crack to be removed. If any nodes are selected prior to the merge, the operation will be limited to those selected nodes. Otherwise the merge operation will apply to all nodes.

Checking Object Dependencies

If the Input class is set to Geometry or Mesh, and an object is currently selected, directly below the input toggles, fields, combo-boxes & options area will be 1) a label box containing the selected object’s type & number and 2) an object associativity list box containing references to the selected object’s dependencies. If the selected object has no object dependencies, then the object associativity list box will read: “No associativity”

For example, selecting a pentahedron element (via the A/O/M configuration of Select > Pentahedron > Selection) will return the selected element’s number (e.g. Element = 73) and the six (6) associated node numbers used to define the element (Nodes = 88,94,87,45,63,44, as shown in Figure 9):

To visually confirm object dependencies, first select the objects of interest. Then click the “Assoc.” button. All objects that depend on the initially selected objects will also be selected.

For more details on object associativity, refer to StressCheck Tutorial: Object Associativity and Why Do I Receive An Error Message About Associativity When Creating or Deleting Geometry?

Standard Element Types

The following standard element types and topologies are available for manual and automatic mesh generation (Figure 10):

• Triangle – A Triangle is an element formed by connecting three nodes which may be used to represent a membrane, an axisymmetric solid or a plate. The nodes may be selected in any order. Triangular elements may be created to represent a three-dimensional shell (thin solid). A triangular element may be also constructed in the 3D reference system in order to construct a pentahedral element by the face to face construction method. If used for this purpose, triangular elements must be deleted from the model before performing an analysis.
• Quadrilateral – A Quadrilateral is defined as an element formed by connecting 4 nodes which may be used to represent a membrane, an axisymmetric solid, a shell or a plate. The nodes may be selected in any order. A quadrilateral element may be constructed in the 3D reference system to represent a 3D shell or in order to construct a hexahedral element by the face to face construction method. If used for this purpose, quadrilateral elements must be deleted from the model before performing an analysis. Note: Create > Quad-Mesh > Auto is capable of generating automeshed quadrilaterals.
• Tetrahedron – A Tetrahedron is defined as an element formed by connecting 4 nodes in the three dimensional reference system. The nodes may be selected in any order. The tetrahedron element may also be constructed by the Face to Face method by connecting an existing triangular element face and one node. Note: Create > Mesh > Auto will generate midside node tetrahedra if in the 3D reference.
• Pentahedron – A Pentahedron is an element formed by connecting 6 nodes in the three dimensional reference system. When constructing the element, you should select them in order by first selecting the nodes which will form one triangular face and then the opposite triangular face. The pentahedral element may also be constructed by the Face to Face method by connecting two existing triangular element faces, or by connecting one quadrilateral face and one edge. Note: Create > Tri-Mesh > Extrude is capable of generating automeshed pentahedra.
• Hexahedron – A Hexahedron is defined as an element formed by connecting 8 nodes in the three dimensional reference system. The nodes may be selected in any order. The hexahedral element may be constructed by the Face to Face method by connecting two existing quadrilateral faces. Note: Create > Quad-Mesh > Extrude is capable of generating automeshed hexahedra.

Manual (Hand) Mesh Generation

Manual (hand) mesh generation requires the selection of existing user-defined nodes, edges or faces. Nodes may be geometrically associative, or not, depending on the node creation method. Below is an animated example of the manual generation of a pentahedron for Create > Pentahedron > Selection:

If the nodes are geometrically associative, then the elements created from those nodes will inherit properties and assignments from the geometry, as well as be geometrically mapped. If the nodes are not geometrically associative, the element edges/faces between these nodes will be faceted. Manual mesh generation methods for standard element types are discussed in Manual Mesh Generation.

MeshSim Automesh Generation

The MeshSim automesh generators are capable of automatically generating meshes of the standard element types, depending on the selected generation method (e.g. Auto, Extrude, Face to Face). A valid sheet or solid body is required for MeshSim automatic mesh generation. Once a valid body is selected, and the desired MeshSim automesh parameters are entered, click the Accept button to create the global automesh record. Then, to generate the automesh, click the Automesh button. Note that as of StressCheck v12.0, it is possible to use manually generated nodes/elements to “seed” the automesh. Below is an animated example of MeshSim automesh generation for Create > Mesh > Auto:

By default, 3D MeshSim automesh generation will result in midside (i.e. quadratically mapped) elements. However, the user may attempt to convert the mapping of these elements to geometric if required for the analysis (e.g. multi-body contact). Automatic mesh generation methods for standard element types by the MeshSim automesher, as well as the influence of the MeshSim automesh input parameters, are discussed in the following:

• MeshSim Automesh Generators
• MeshSim Automesh Generation Methods
• What Do the MeshSim Global Automeshing Parameter Inputs Affect?

Special Mesh Objects

Several special mesh objects are available for specific theories/analyses, such as beam theory, fastened connections, multi-body contact, and 2D crack path analysis (Figure 11):

• Beams – A beam is defined by selecting two nodes in any order. The order in which the nodes are picked when creating the elements defines the principal directions of the beam. The beam axis is defined in the direction from the first to the second node. A beam element cannot be used in conjunction with other element type. Beam elements can be used in Planar and 3D Elasticity.
• Fasteners – A Fastener is a special element that can be attached to circular boundaries. It consists of a rigid core with two degrees of freedom connected to the planar body by a distributed radial (normal) spring. The rigid core can be connected to the rigid core of other fasteners directly or using a link element, it can be fixed in one or both directions, or it can be loaded by a force or an imposed displacement. Learn more about fastener elements in Fastened Connection Analysis Overview.
• Links – Under planar elasticity, a Link is a special element to connect fastener elements allowing the simulation of the shear/bending stiffness of the fastener. Under 3D elasticity, links are created to connect contact zones representing a shell/solid connection. Learn more about link elements in Fastened Connection Analysis Overview.
• Contact Zones – A Contact Zone is a special mesh object identifying the surfaces/faces in 3D, or curves/edges in 2D, where contact is expected to be computed. Note: at least two contact zones must be created for each potential contact pair. Contact pairs are assigned as constraints (Select > Contact Zone > Contact). Learn more about contact zones in Multi-Body Contact Overview.
• Cracks – A Crack is a special mesh object used in 2D Crack Path analysis. A crack may be activated and extended using the Crack Path solver. Learn more about crack objects in Crack Path Analysis Overview.

Selecting/Editing Mesh Objects

So far, we have described how to create mesh objects by setting the Action combo-box to Create. It is very important to be able to select, manipulate, edit, examine and/or update mesh objects/automesh generators after they have been created. The Action combo-box of the C/A/O/M combo-boxes in the Mesh input class contains the following additional actions:

• Select – selection of objects from the screen.
• Edit – selection of an object from the screen or the Data subtab’s Object Identifier (OI) listbox for revision of input data.
• Move To – selection of an object from the screen for redefinition of the creation method and/or input data.
• Check – selection of an object (e.g. node) to query properties like location/dimensions/distance from another object, or to query the distortion/area/volume of an element, group of elements or the mesh.

Additionally, when the Action is set to Select or Edit two buttons are available at the bottom of the Input dialog for revising selected objects:

• Move – increment object location/dimensions.
• Replace – overwrite object location/dimensions.

These actions are summarized as follows:

Select

Set the Action combo-box to Select to identify an object for manipulation by some other command. You may then set the Object combo-box to the desired mesh object type (e.g. Node, Quadrilateral, Tetrahedron, Contact Zone). Each time you select an object from the Model View, the location and dimension information will appear automatically in the input fields which have been set for screen input. If a field has been set for manual data input, the current manual input data will be retained.

Figure 12 shows the location information from the selection of a node via Select > Node > Selection:

By default, each selection operation automatically cancels the selection of other objects. Pressing the Shift key while selecting an object will enable the selection of multiple objects. Pressing the Ctrl key will allow you to cancel a particular selected object without affecting other selected objects. The Cancel Highlighted Objects icon in the Edit Toolbar or right-clicking in the Model View may be used to cancel all selected objects, regardless of type. The Cancel Specific Object Type icon in the Edit toolbar may be used to cancel the selection of all objects of the current object type.

Note: the coordinate location is always given in global coordinates when using Select. Set the Action combo-box to Edit to obtain actual input definitions of an object. See the discussion below on the use of the Replace and Move buttons with objects which have been selected.

Edit

Set the Action combo-box to Edit to identify an object so that you may examine and/or revise its definition. You may then set the Object combo-box to the desired mesh object/automesh generator type (e.g. Node, Any Element, Mesh, Contact Zone). Select an object from the Model View or the Object Identifier (OI) listbox under the C/A/O/M, and the input fields associated with the selected mesh object/automesh generator type and creation method will appear in the Input dialog. Note: automeshed nodes/elements will not be accessible via the OI listbox; use the the Index subtab’s grid control to access the details of these mesh objects.

An example OI list for hand-meshed node objects is shown below in Figure 13:

Once the object is selected for edit, the OI listbox status will show the object as “Selected” and the current object data will appear automatically in the greyed-out input fields which have been set for screen input. If a field has been activated for manual data input, the current manual input data will be retained during object editing.

To revise the mesh object/automesh generator data associated with an input field, enable the checkbox next to the input field and modify the input data. Then, you may click the Replace or Move button (see the discussion below on the use of the Replace and Move buttons for an object being edited). For example, if you Edit a node defined at a parametric Global location via Edit > Node, the input fields will populate with that node’s X, Y, Z values (Figure 14):

Enable the checkbox next to the X: input field (current value is Tlug/2), and enter a new value (Tlug/2*100). Then, click Replace to revise the node definition.

If the object is associative then those objects on which it depends are also highlighted in the Model View. For example, if you Edit a node defined as an intersection (Method: Intersection), the two intersecting boundaries will be highlighted and listed in the Input dialog to indicate the associativity condition (Figure 15):

Note: when you select the object on the screen or from the OI listbox, the method by which the object was originally defined will appear in the Input dialog. You should not change the method when using Edit. Use Move To for this purpose.

Move To

Set the Action combo-box to Move To to change the definition of an existing object while keeping its object number intact. This action is intended for direct manipulation of an object with the mouse cursor. When you edit the object, it will be highlighted, and the method by which the object was created will be highlighted in the Method combo-box. Additionally, the mouse cursor will change to the Create cursor ().

To revise the definition of the object, simply redefine it as though it were a new object. You may change the creation method (such as switching from Projection to Offset), select new associative objects from the Model View (such as selecting new nodes for an element), and/or supply new coordinate or dimension information manually in the input fields. When you are ready to apply your changes, click the left mouse button in the Model View, or click the Replace button. Using the Replace button will preserve any coordinate or dimension information from the original object definition corresponding to input fields which are turned off.

The following animated example shows how Move To was used to revise the definition of a node from the Intersection method to the Offset method:

Note: if you use the cursor to activate the revision, the appropriate coordinate, dimension, or associativity information will be determined by the proximity of your cursor pick location.

Check

Set the Action combo-box to Check to perform various query operations on mesh objects. Check may be used to obtain object definition information, to compute the location of a node, to compute the distance between two nodes, to check for free edges between elements, to compute the min/max solid angles of elements (i.e. element distortion), or to compute area/volume properties of elements.

Locate

Set the C/A/O/M to Check > Node > Locate and select a node to return its location in Global coordinates.

Distance

Set the C/A/O/M to Check > Node > Distance and select any two nodes to return the distance between the two nodes.

Free Edge/Face

This feature is very useful for determining whether there are any cracks or improperly connected regions in manually or automatically meshed models. Set the C/A/O/M to Check > Edge > Free Edge and all free element edges will be selected and highlighted automatically; similarly, Check > Face > Free Face may be used to highlight free element faces in 3D meshes.

Note: for 3D meshes, the Mesh Transparency toggle may be useful for visualizing free element faces, especially for embedded 3D crack fronts.

Distortion

Set the C/A/O/M Action to Check, the Object to the desired element type (Any Element, All Elements, Mesh, Triangle, Quadrilateral, Tetrahedron, Pentahedron or Hexahedron), and the Method to Distortion. Then, if desired, set the minimum acceptable solid angle (MinAng) and/or maximum acceptable solid angle (MaxAng) values in degrees. If applicable select the element or elements, and click Accept. A tab above the Model View will appear with a report on element distortion.

If any elements are flagged as distorted based on the input vertex angle criteria (MinAng, MaxAng), they will automatically be added to an element set with the name “DISTORT_WARN” for further inspection.

Note: StressCheck’s element implementation is less susceptible to element distortion. By default, an element is flagged as distorted if 5 > Vertex Angle > 175. If you wish to override the default valid angle range, simply enter the values in the MinAng and MaxAng input fields. The smallest vertex angle accepted for an element is zero degrees and the maximum is 179 degrees. An element with a vertex angle greater than 179 degrees will be rejected, and the execution will not be performed until the element is modified.

Properties

Set the C/A/O/M Action to Check, the Object to the desired element type (Any Element, All Elements, Mesh, Triangle, Quadrilateral, Tetrahedron, Pentahedron or Hexahedron), and the Method to Properties. If applicable select the element or elements, and click Accept. A tab above the Model View will appear with a report on element properties. The property check will return area/cross-sectional properties in 2D (Planar), and volume/centroidal properties in 3D.

If there is a failure during the computation of any element properties, these elements will be marked as illegal and will automatically be added to an element set with the name “DISTORT_FAIL” for further inspection. Note: while distorted elements can be passed to the solver, illegal elements cannot and must be evaluated/re-meshed.

Replace and Move Buttons

The Replace and Move buttons can be used to change the definition of all selected objects. If you have identified an object using the Select, Edit, or Move To actions, you may manually change for example a coordinate or MeshSim parameter value in the input area using the Replace or Move buttons.

• Replace will change the coordinate or dimension of the selected object to the one given.
• Move will increment the coordinate or dimension by the magnitude given in the input field.

Only the coordinate or dimension values selected for manual entry will be affected during the Replace or Move operation. For example, if you select 5 different global nodes, then turn on only the X: coordinate input toggle and enter a new value, a Replace operation will assign the same X coordinate to all nodes whereas a Move operation will translate all selected points by the magnitude of the value in the X: coordinate input field.

Hiding/Showing Mesh Objects

To hide objects from the Model View temporarily, use the Select action to identify the object(s) to be hidden and then use the Hide Objects icon in the Edit Toolbar, Display > Selection > Hide from the main menu, or the Hide option in the right-click context menu. The selected objects will then be hidden from the Model View. To restore (unhide) the hidden objects, click on the Unhide Objects icon in the Edit Toolbar, Display > Selection > Unhide from the main menu, or the Unhide option in the right-click context menu. The hidden objects will then be displayed in the Model View.

For more information on hiding/showing objects, refer to How Do I Use the Edit Toolbar to Select, DeSelect, Blank and Unblank Objects?

Deleting Mesh Objects

There are several ways to delete mesh object/automesh generator records from within the Mesh tab:

• Screen selection of objects in the Model View, then clicking the Delete button.
• Selection of an object/automesh generator record or records from the Index subtab scrolling list, then clicking the Delete button.
• Selection of a specific object/automesh generator record from the Data subtab’s OI listbox under the C/A/O/M combo-boxes when Action is set to Edit, then clicking the Delete button.
• Clicking the DeLast button.

When Action is set to Select and the Object combo-box is set to “Any Object” in the C/A/O/M combo-boxes, then any object type can be selected for deletion. To select and delete objects of a specific object type, such as quadrilaterals, set the Object combo-box to the object type you wish to delete (in this case, “Quadrilateral”). Then, only quadrilateral elements can be selected and deleted.

If attempting to delete objects from a model, it may be necessary to first delete objects that have associative relationships that depend on the object that you wish to delete. To determine object dependencies, first select the objects of interest. Then click the “Assoc.” button. All objects that depend on the initially selected objects will also be selected. At this point you may perform the Delete operation. Note: if an error appears related to associativity, it may be necessary to use the Assoc. button to determine object dependencies.

Note: if you delete an object by mistake, select Edit > Undo from the Main Menu Bar or use the Undo button in the Edit Toolbar to retrieve the deleted object. More on DeLast vs. Undo in the following.

Screen Selection

First, in the C/A/O/M combo-boxes set Action to Select and the Object combo-box to the desired mesh object type (e.g. Node, Quadrilateral, Tetrahedron, Contact Zone). Left-click on an object in the Model View, or hold the Shift key and left-click on multiple objects, or marquee select a group of objects by left-click + drag, to highlight the object(s) to be deleted. Then, click Delete to remove the object(s).

If selecting a single object of a specific object type for deletion, then you may also set Action to Edit and select an object in the Model View. The object can now be deleted by clicking the Delete button.

Index Subtab List Selection

First, in the C/A/O/M combo-boxes set Action to Select and the Object combo-box to the desired mesh object/automesh generator type (e.g. Node, Mesh, Tetrahedron, Contact Zone). Then, change from the Data to the Index subtab. A scrolling numbered list containing mesh objects/automesh generators of the selected object/automesh generator type (or all objects if the Object combo-box was set to “Any Object”) will appear. Left-click on the list items you wish to delete, then click the Delete button.

If selecting a single object of a specific mesh object/automesh generator type for deletion, then you may also set Action to Edit and select an object from the scrolling list. The object can now be deleted by clicking the Delete button.

Data Subtab OI Listbox Selection

In a similar way that an object can be edited/replaced, in the C/A/O/M combo-boxes first set Action to Edit and the Object combo-box to the desired mesh object/automesh generator type (Node, Mesh, Tetrahedron, Contact Zone). An OI listbox containing records of the selected object/automesh generator type will appear under the C/A/O/M combo-boxes. Then, you may select the record you wish to delete from the OI listbox, and then click the Delete button.

DeLast Button

If you wish to delete the last mesh object/automesh generator created, simply click the DeLast button to the right of the Delete button. The object will be removed from the screen, the OI listbox on the Data subtab if Action to Edit, and the scrolling listbox in the Index subtab. Note: if the last object generated was an automatic mesh, all automatic mesh objects will be deleted.

DeLast vs. Undo

The DeLast button can be very useful to retrace several creation operations. But, be aware that DeLast is NOT the same as an Undo operation. It only deletes the last object created. Once an object is deleted, it can be recovered using Undo. Repeating DeLast will continue to delete objects in the reverse order of creation until all objects have been deleted.

StressCheck also provides an Undo operation. Undo reverses the outcome of the previous object or data operation. If an object was created, Undo will remove the object. If an object was deleted, Undo will recover the deleted object. If an object was moved, the object will be returned to its original location. Undo does not have any effect on display operations such as rotation, translation, selection, cancellation, etc.

Note: If your session contains data from a finite element solution, this data will be destroyed by an Undo operation. After an Undo operation, the Redo operation will reverse the effect of the Undo. The Undo can be repeated to retrace all object or data related operations back to the start of the current StressCheck session. Redo can be used to reverse all Undo operations. As soon as a new operation is requested other than an Undo, the possibility of a Redo is eliminated.

For more information on DeLast vs Undo, refer to What’s the Difference Between DeLast and Undo?

Example: Editing & Deleting an Automatic Mesh Record

In some cases where the default automesh settings are not sufficient, it may be necessary to edit or delete a previously created global automesh record. The Parasolid file for the following example may be downloaded here.

Creating a Global Automesh Record

As discussed above under “MeshSim Automesh Generation”, to create a global automesh record for a sheet or solid geometry, set the A/O/M in the Mesh tab to Create > Mesh > Auto and then select the body to be automeshed. The body will highlight red. Then, click the Accept button to create the global automesh record.

To generate the automesh, click the Automesh button. The default automesh settings were used to generate the below mesh:

Editing a Global Automesh Record

To modify the automesh settings for a global automesh record, simply select the global automesh record from the OI listbox under the A/O/M, check the global automesh setting(s) to be replaced, update the inputs(s), and then click the Replace button.

To re-generate the automesh, click the Automesh button. The global automesh setting D/H was modified from the default (0.114) to 0.05 and the mesh was re-generated with the new global automesh settings:

Deleting a Global Automesh Record

To delete a global automesh record, and remove all automeshed elements for that geometry, simply select the global automesh record from the OI listbox under the A/O/M and click the Delete button. The global automesh record and the mesh will be deleted:

Was this article helpful?

0.5 out Of 5 Stars

1 rating

5 Stars		0%
4 Stars		0%
3 Stars		0%
2 Stars		0%
1 Stars		100%

5 Submit

How can we improve this article?

Please submit the reason for your vote so that we can improve the article.

Submit